If you just want to rapid to your Zero position, this is happening in your first program here:
N850G00X0.000Y0.000
You can alter your post in RhinoCam to add this in the end of the program, or the end of each tool.
Hi
I am used to generating gcode from Vetric software but though i’d try out Rhinocam. I ran the same pocketing toolpath in both software to compare. I’m used to the the tool retracting to safe Z and then returning to zero’d position but remaining at the safe z. Rhinocam retracted to safe z didn’t move to zero’d position. I wonder what instruction to add to the Rhinocam Mach 3 post processor to give it the instruction to move to job zero position, see gcode.
Any thoughts on this would be most useful.
Thanks
————————————————� �———————————————
Aspire
(Toolpaths used in this file
(aspire 150x75 Roughing)
(Tools used in this file: )
(1 = End Mill {6 mm} roughing wood)
N100G00G21G17G90G40G49G80
N110G71G91.1
N120T1M06
N130 (End Mill {6 mm} roughing wood)
N140G00G43Z20.000H1
N150S12000M03
N160(Toolpath:- aspire 150x75 Roughing)
N170()
N180G94
N190X0.000Y0.000F3600.0
N200G00X86.445Y-162.500Z5.000
N210G1Z0.020F1200.0
N220G1Y-12.500F3600.0……………….
Middle gcode removed
N800G1Y-162.500
N810G1X14.445
N820G1Y-12.500
N830G00Z5.000
N840G00Z20.000
N850G00X0.000Y0.000
N860M09
N870M30
%
————————————————� �———————————————
Rhinocam
G00 G49 G40.1 G17 G80 G50 G90
G21
(Horizontal Roughing)
M6 T3
M03 S12500
G00 Z6.0000
X87.5000 Y-162.5000
G01 Z-1.7650 F4000.0
Z-2.4000 F1500.0
Y-12.5000 F3600.0
X85.1000
Y-162.5000
X82.7000
Y-12.5000
X80.3000
Y-162.5000
X77.9000
Y-12.5000
X75.5000……………….
Middle gcode removed
Y-162.5000
X12.5000
Y-12.5000
Z-1.7650 F3000.0
G00 Z6.0000
M5 M9
M30
————————————————� �———————————————
Similar Threads:
If you just want to rapid to your Zero position, this is happening in your first program here:
N850G00X0.000Y0.000
You can alter your post in RhinoCam to add this in the end of the program, or the end of each tool.
Thanks,
The Mach3 post in Rhino is giving me these option on start/stop.
Excuse my ignorance* but is it all or part of 'N850G00X0.000Y0.000' to add to the end?
*I really should have learnt more about G commands before launching into the world of cnc.
[START_CHAR]
[SEQ_PRECHAR][SEQNUM][DELIMITER]G00 G49 G40.1 G17 G80 G50 [OUTPUT_MODE_CODE]
[SEQ_PRECHAR][SEQNUM][DELIMITER][OUTPUT_UNITS_CODE]
[SEQ_PRECHAR][SEQNUM][DELIMITER]M5[DELIMITER]M9
[SEQ_PRECHAR][SEQNUM][DELIMITER]M30
[STOP_CHAR]
[SEQ_PRECHAR] puts the N in the line.
[SEQNUM] puts the actual line number after the N.
[DELIMITER] adds a space in this instance, but can be changed to other characters if needed. (The space appears to be fine at the moment)
Try the following:
Moving to your zero position may be what you want here, but more commonly machines are sent to the "Home" position at the end of a program which is often performed by a "G28" line. Do what works for you though.Code:[SEQ_PRECHAR][SEQNUM][DELIMITER]M5[DELIMITER]M9 [SEQ_PRECHAR][SEQNUM][DELIMITER]G00[DELIMITER]X0.0000[DELIMITER]Y0.0000 [SEQ_PRECHAR][SEQNUM][DELIMITER]M30 [STOP_CHAR]
Thanks a lot!
Yes correct, I want to move to my zero position. I'm just off to the workshop now so i'll try this out.